First time PCB designer, so I have no practical experience. I have all the parts for a small personal project. And, I have created footprint packages for all the unique components I plan to use. I used drill sizes in my footprint packages that fit the actual sizes I measured from the parts. It seemed the correct thing to do. I just need some confirmation. For example, here are a couple of the cases, just to draw a picture:
capacitor, leads are actual 31.4 mils, I used a drill size 31.496 (Eagle)
capacitor, leads are actual 23.5 mils, I used a drill size 23.622
LED, leads are actual 21.0 mils, I used a drill size 23.622.
In the first two cases, above, the component leads are right there, right at the drill size. In the last case, the leads are a little smaller than the next drill size up.
I do not know whether there needs to be any extra allowance where the hole should measure to the next drill size above a a standard wire size.
Like I said, I have all the component packages in my own libraries and i can change the values to what would be “perfect” for this one case.
You need more clearance around the leads, so that the solder can flow into the hole properly, and to make assembly easier. You should also use standard drill sizes.
If you’re getting a solder finish on your PCBs (as opposed to gold etc), then you might want to allow for bigger sizes again. I found this out the hard way with a batch of PCBs from Gold Phoenix (we had to use a press to insert one of the connectors).
Thanks for the responses. Looks like I will need to do some more research. I have time before I need to explore the finer details of the board finishing. This little project gets more complex as I move along.
First time PCB designer, so I have no practical experience. I have all the parts for a small personal project. And, I have created footprint packages for all the unique components I plan to use. I used drill sizes in my footprint packages that fit the actual sizes I measured from the parts. It seemed the correct thing to do. I just need some confirmation. For example, here are a couple of the cases, just to draw a picture:
capacitor, leads are actual 31.4 mils, I used a drill size 31.496 (Eagle)
capacitor, leads are actual 23.5 mils, I used a drill size 23.622 LED, leads are actual 21.0 mils, I used a drill size 23.622.
In the first two cases, above, the component leads are right there, right at the drill size. In the last case, the leads are a little smaller than the next drill size up.
I do not know whether there needs to be any extra allowance where the hole should measure to the next drill size above a standard wire size.
Like I said, I have all the component packages in my own libraries and i can change the values to what would be “perfect” for this one case.
Bill M
Use a drill size that is 8mil - 10mil larger than your lead size. Round this value up to the nearest whole number. For example, for your 31.4 mil leads, use a 42 mil drill (or 1.1mm). BTW, a 40mil (or 1.0mm) drill works great for a 25mil square lead.
Thank you. I had been thinking that my original question was too vague and I was about to ask for some additional detail. Your response addressed my issue. I am in uncharted territory here. I never worked with surface mount components and I never had someone else manufacture a PCB for me. This little personal project of mine has me using all the tricks I know and now some more. I can work with your rule-of-thumb. Thanks again.
In general I agree with Dave’s rule-of-thumb, but with the rider that the actual oversize amount relate to the actual lead size i.e. use more when dealing with bigger leads, less when dealing with tiny leads. However, there are more things to consider, and it’s better to be aware of them up front than to learn through hard experience.
Find a good board manufacturer, get experience with them, and stick with them. Not all manufacturers are created equal!
Here are a couple of points to keep in mind. I’m sure there are dozens of others that could be added. Also, have a look at the IPC site, and have a close look at the specifications (abilities) of your board manufacturer.
Benefits of larger holes.
Allows some flexibility in your component selection - a second-source item may have slight differences to the original that you designed around.
Apart from making it easier to install, it makes it a lot easier to remove if you need to.
Component lead spacing is not always perfect. Small parts are generally pretty close to spec, and consistent. Large items, especially packaged/potted items may have significant variations.
Drawbacks of larger holes.
Parts tend to fall out when you invert the board for soldering. That can be overcome by bending a couple of leads over, but that can lead to difficulties (and track/via damage) if the part ever needs to be replaced. The larger the clearance the more awkward it can be to hold a component in place correctly for soldering.
As a special case of (1.), mating components (connectors) soldered individually to two boards can be significantly mis-aligned when it comes time to mate the boards. For a given ‘oversize’ amount, this effect will be less noticable with long connectors, but that same oversize amount can cause grief when short connectors on two boards become badly mis-aligned.
Depending on the particular component pads and adjacent trackwork, making the hole larger may restrict the size of the pad annulus. When that is combined with a board manufacturer who has poor registration between drilling the holes and printing the artwork, you can run into problems during initial assembly, and even worse problems during rework.
Thank you. More words of wisdom, to live by. They make sense and I will fold them into my plans. I appreciate the effort you put into your response. Others can benefit from the advice as well.
What you offered about the 25mil square lead is interesting. It begs another beginner question. Bear with me.
I am using Eagle software. The “standard” drill sizes that Eagle lists for a component range in mils, for example, from .027559, .031496, .035433, .03937 to .043307. I could manually override any drill size in Eagle and add a new value at 42 mils, but I could not say that such a drill size is “valid”. As a beginner, I am assuming that drill bits come in standard sizes, as listed by Eagle. In the CNC world, I do not know how a hole is drilled or sized to a dimension and what my limits are to specify an “odd” size, since 40 mils does not fit the Eagle “template”. It is in between the standard drop down menu values of .03937 and .043307. I have a metal working lathe in the garage, so I am comfortable working with small numbers and close tolerances, but I am not a CNC guy.
Can you illuminate me?
Bill M
[/quote]
Use a drill size that is 8mil - 10mil larger than your lead size. Round this value up to the nearest whole number. For example, for your 31.4 mil leads, use a 42 mil drill (or 1.1mm). BTW, a 40mil (or 1.0mm) drill works great for a 25mil square lead.
It seems that most PCB places will just pick the closest standard drill size for each hole, assuming the hole is between their min and max specification (ie, your hole diameters don’t have to exactly match what’s in their drill rack).
Most places don’t actually tell you what their standard drill rack is; Olimex is one exception - they have a fairly limited number of standard drill sizes, and charge extra for any holes that aren’t very close to one of these sizes.